Download CIMCO CNC-Calc 2 - User Guide with tutorials 1-10

1
2
3
CIMCO CNC-Calc 2.5 User Guide
© 1991 - 2010 CIMCO Integration - May 14, 2010
4
5
2. License information
Information in this document is subject to change without notice and does not represent a
commitment on the part of CIMCO Integration. The software described in this document
may be used or copied only in accordance with the terms of the license. The purchaser
may make one copy of the software for a backup, but no part of this user manual may
be reproduced, stored in a retrieval system, or transmitted in any form or by any means
electronic or mechanical, including photocopying and recording for any purpose other than
the purchaser’s personal use, without prior written permission from CIMCO Integration.
TERMS OF USE FOR:
Software: CNC-Calc v2
Version: 2.x.x
Date: January 2010
Copyright (c) 2010 by CIMCO Integration
Notice:
CIMCO Integration reserves the right to make changes to the CNC-Calc v2 Software at any
time and without notice.
Software License
You have the right to use the number of licenses of the enclosed program, which you have
bought from CIMCO Integration. You may not distribute copies of the program or related
documentation to any persons or companies. You may not modify the program or related
documentation without the prior written consent of CIMCO Integration.
Disclaimer of all Warranties and Liability
CIMCO Integration makes no warranties, either express or implied, with respect to the
software, its quality, performance, merchantability, or fitness for any particular purpose.
The entire risk as to its quality and performance is with the buyer. Should the CNC-Calc
v2 software prove defective following its purchase, the buyer (and not CIMCO Integration,
its distributor, or its retailer) assumes the entire cost of all necessary servicing, repair, of
correction and any incidental or consequential damages. In no event will CIMCO Integration
be liable for direct, indirect, or consequential damages resulting from any defect in the
software, even if CIMCO Integration has been advised of the possibility of such damages.
Some jurisdictions do not allow the exclusion or limitation of implied warranties or liability
for incidental or consequential damages, so the above limitation or exclusion may not apply
to you.
6
Notice:
The accompanying software is confidential and proprietary to CIMCO Integration. No use
or disclosure is permitted other than as expressly set forth by written license with CIMCO
Integration.
Copyright (c) 2010 CIMCO Integration. All rights reserved.
THIS SOFTWARE CONTAINS CONFIDENTIAL INFORMATION AND TRADE
SECRETS OF CIMCO INTEGRATION. USE, DISCLOSURE, OR REPRODUCTION IS
PROHIBITED WITHOUT THE PRIOR EXPRESS WRITTEN PERMISSION OF CIMCO
INTEGRATION.
The CIMCO Logo is a trademark of CIMCO Integration. Microsoft, Windows, and Windows
NT are registered trademarks of Microsoft Corporation. Other brand and product names are
trademarks or registered trademarks of their respective holders.
Contacting CIMCO Integration
Address:
CIMCO Integration I/S
Lundtoftegaardsvej 97, 3.
DK-2800 Lyngby
Denmark
Phone: +45 4585 6050
Fax: +45 4585 6053
E-mail: [email protected]
Web: http://www.cimco-software.com
7
8
3. Table of Content
4.
Installation 9
5.
Overview 10
6.
Mouse functions 12
7.
Toolbars 13
8.
Menus 23
9.
Configuring CNC-Calc 32
10.
Color configuration 36
11.Other configurations that affect CNC-Calc 37
Milling tutorials
12.Tutorial 1 2D Construction 38
13.Tutorial 2 CNC-toolpaths and Face milling 48
14.Tutorial 3 Contour milling 57
15.Tutorial 4 Pocket milling 67
16.Tutorial 5 Backplot in the Editor 77
17.Tutorial 6 Drilling 84
18.Tutorial 7 Milling of Letters 89
19.Tutorial 8 Milling of TrueType Letters 96
Turning tutorials
20.Tutorial 9 Drawing the part 105
21.Tutorial 10 Machining the part 119
9
4. Installation
CNC-Calc v2 is installed as part of CIMCO Edit v5. Please see the CIMCO Edit v5
documentation for installation instructions.
If you are upgrading an existing installation without CNC-Calc v2 you do not need to
reinstall CIMCO Edit v5. Just copy the new keyfile (named “license.key”) to the appropriate
directory.
10
5. Overview
CNC-Calc v2 can draw 2D geometry, and generate NC code in ISO and Heidenhain
conversational format for contours and drilling cycles. The main program window looks like
this (with an empty drawing pane):
The toolbars can be arranged as desired by dragging them around. They can be docked along
any edge of the program window, in any order, or they can be placed floating on top of the
program window or outside the program window.
To the left of the drawing pane, you see the CNC-Calc
and Element Inf o panes. The CNC-Calc pane shows
coordinate entry fields and other information about the
activity you are performing at any given time, while the
Element Info pane shows the statistics of the element you
are hovering the mouse over. To the right, you can see an
example of the Element Info pane display.
11
Most of the functions in CNC-Calc v2 can be accessed through toolbars and the CNCCalc menu, though a few functions are accessed in the File menu in CIMCO Edit v5 . The
following sections will first describe the mouse functions, then the toolbars and menus.
12
6. Mouse functions
The mouse buttons are used to perform the following functions:
Left button Selects whatever is described in the lower left corner of the
program window.
Middle button (on most mice, pressing the scroll wheel)
Fits/zooms the geometry drawing to the entire graphics area.
This can also be achieved by clicking the icon.
Right buttonDrag the geometry drawing across the graphics area by holding
down the right mouse button as you drag the mouse.
Scroll wheel Zoom in and out, centered on the cursor position.
13
7. Toolbars
7.1. Tool
The Tools toolbar handles file operations, toolpath functions, zoom, snap and configuration
access. The functions in the Tools toolbar are also available from the CNC-Calc menu.
New Drawing clears the graphics area (you will get a chance to save
any unsaved changes). This can also be accessed with Ctrl N.
Open Drawing opens existing CNC-Calc v2 or DXF files. This can
also be accessed with Ctrl O. The downwards arrow next to the open
icon gives access to a recent files list, making it easy to reopen a file
which you have been editing recently.
Save saves the drawing to your hard disk. If it is the first time you
save the drawing, you will be prompted for a file location and name.
Save can also be accessed with Ctrl S.
Zoom in centered on the middle of the graphics area. Zoom in can
also be accessed with Page Down.
Zoom out centered on the middle of the graphics area. Zoom out can
also be accessed with Page Up.
Zoom All fits the drawing to the graphics area. This can also be done
by clicking the middle button on the mouse (on most mice, pressing
the scroll wheel), or with Ctrl-End.
Zoom Window lets you zoom in on an area, which you select by first
clicking at one corner, then dragging the rectangle and clicking at the
opposite corner.
14
Snap to Grid snaps to the grid points.
Snap to Points snaps to points drawn by the user.
Snap to Center Points snaps to the centers of circles and arcs.
Snap to Mid points snaps to the midpoints of elements.
Snap to Mid points snaps to the midpoints of elements.
Snap to Intersections snaps to the intersections between elements.
Enable All Snap Types activates all snap types.
Disable All Snap Types deactivates all snap types.
Setup CNC-Calc lets you access the configuration for CNC-Calc.
7.2. Points and Lines
The Points/Lines toolbar contains functions for drawing lines and points defined in different
ways. The functions in this toolbar can be found under Draw Points/Lines in the menu.
Setup CNC-Calc lets you access the configuration for CNC-Calc.
Between 2 Points will draw a line between two selected points.
Vertical will draw a vertical line. The first point selected defines
the starting point (and the X coordinate), the second point selected
defines the length (and need not be directly above or below the first
point).
15
Horizontal will draw a horizontal line. The first point selected
defines the starting point (and the Y coordinate), the second point
selected defines the length (and need not be directly to the left or
right of the first point).
Polar lets you select the starting point of a line, and you then select
(or write) the angle and length of the line.
Perpendicular draws a line perpendicular to another line. You first
select the line your new line is to be perpendicular to, then the
starting point of your new line. You then select the length of your
new line, and last you select in which direction from the starting
point your new line is to go.
Parallel draws a line parallel to another line. You first select the line
your new line is to be parallel to, then the starting point of your new
line. You then select the length of your new line, and last you select
in which direction from the starting point your new line is to go.
Bisector draws a line bisecting two other lines, i.e. a line that halves
the angle between two lines. You first select the two lines you want
to bisect, then you select the length of your new line (from the
intersection of the two lines you are bisecting), and last you select
which of the four possible solutions you want to keep.
Tangent Two Elements lets you draw a line tangent to two circles or
arcs. You select the two circles or arcs your new line is to be tangent
to, and then you select which of the solutions you want to keep.
Tangent Angle draws a line tangent to an arc or circle, at a selected
angle. You first select the arc or circle your new line is to be tangent
to, then the angle and length, and last you select which of the two
solutions you want to keep.
Tangent Through Point draws a line tangent to an arc or circle, to a
selected point. You first select the arc or circle your new line is to be
tangent to, then the point it is to go though, and last you select which
of the two solutions you want to keep.
16
Rectangle draws a rectangle where you select the two opposite
corners. It is possible to define a corner radius for the rectangle (the
corner radius is ignored if there is not room for it).
7.3. Arcs and Circles
The Arcs/Circles toolbar lets you draw full circles (360 degree arcs), arcs and bolt patterns.
The functions in the Arcs/Circles toolbar can be found under Draw Arcs / Circles and Draw
Special in the menu.
Center Radius lets you define the center of the circle, followed by
the radius.
Two Points lets you define the circle by selecting two (diametrically
opposite) points.
Three Points lets you define the circle by selecting three points on
the periphery of the circle.
Center Diameter lets you define the center of the circle, followed by
the diameter.
Tangent Two Elements lets you define a circle tangent to two
elements, of a defined radius. You first write the radius, then you
select the two elements the circle is to be tangent to. Last you select
which of the solutions you want to keep.
Tangent Center on Line lets you define a circle tangent to one
element, with its center on a line, of a defined radius. You first write
the radius, then you select the line the center is to be on, and the
element the circle is to be tangent to. Last you select which of the
solutions you want to keep.
17
Tangent through Point lets you define a circle tangent to one
element, through a point, of a defined radius. You first select the
point the circle is to go through then write the radius, and select the
element the circle is to be tangent to. Last you select which of the
solutions you want to keep.
Tangent Three Elements defines a circle tangent to three elements.
You select the three elements the circle is to be tangent to, and then
you select which of the solutions you want to keep.
Two Points lets you draw an arc by selecting the endpoints of the
arc, entering the radius, and selecting which solution you want to
keep.
Three Points lets you draw an arc by selecting three points. Note,
that the arc created will not cross the zero degree point (3 o’clock);
The order the three points are selected in does not matter.
Start and End Angles lets you define an arc by its center point,
radius, starting angle and end angle.
Rectangular Bolt Hole Pattern defines a rectangular bolt pattern. You
select the start point (one of the corners), and then enter the step in
X, step in Y, number of holes in X, number of holes in Y and the
hole diameter.
Circular Bolt Hole Pattern defines a circular bolt pattern. You select
the center of the bolt pattern, select the radius of the bolt pattern, and
then enter the start angle, step angle, number of holes and the hole
diameter.
18
7.4. Letters
The Letters toolbar lets you draw two kinds of letters; simple letters and True Type letters.
The simple letters are like the letters used on drawings. These letters can be used to mill, for
instance, a part number on a part. The True Type letter is more artistic, and any True Type
font installed in the Windows operating system can be used. The Letters toolbar can be found
under Draw Arcs / Circles and Draw Special in the menu.
Simple Text Linear Alignment defines simple text written on a line.
You enter the starting point, angle of the line, then the distance
between and height of the letters. It is also possible to select the
horizontal and vertical alignment of the text.
Simple Text Circular Alignment defines simple text that is written
on a circle. You select or enter the center and radius of the alignment
circle, then the start angle, space between and height of the letters. It
is also possible to select the horizontal and vertical alignment of the
text, on the circle.
True Type Text Linear Alignment defines True Type text written on
a line. You enter the starting point and angle of the line, and then the
height of the letters. It is also possible to select the horizontal and
vertical alignment of the text.
True Type Text Circular Alignment defines True Type text that is
written on a circle. You select or enter the center and radius of the
alignment circle, then the start angle and height of the letters. It is
also possible to select the horizontal and vertical alignment of the
text, on the circle.
19
7.5. Modify
The Modify toolbar modifies the geometry in different ways. The functions in the Modify
toolbar can be found under Modify in the menu.
Trim To Intersection will trim the selected element to the nearest
intersection(s). Select the element to be trimmed on that part to be
removed; It is then trimmed to the intersection(s) nearest the point
where it was selected. The trimmed element is also broken in two, if
there are intersections on both sides of the selected point.
Trim One Element will trim one element to another. Select the
element to be trimmed first, on the side to be kept, and then select
the element to trim to.
Trim Two Elements will trim two elements to each other. Select the
two elements to be trimmed, on the side to be kept.
Fillet Elements creates a fillet between two elements, with a fillet
radius the user selects. It is optional whether the two elements
should also be trimmed to the fillet.
Break Elements will divide an element into two pieces. First select
the element to be broken into two, and then select the point at which
it should be divided.
Join Elements will join two selected elements into one.
Delete will delete the elements you select. They can be restored with
the Undo function (the icon or Undo under Modify in the menu.
Offset Elements will offset the elements you select by a specified
distance. It is optional whether the original element should be kept.
20
Mirror Elements will mirror the elements you select about a line
selected as the mirror axis.
Translate Elements will translate the elements you select along a
vector defined by selecting two points. It is optional whether the
original should be kept, and it is possible to create multiple copies,
where each copy is translated one step further along the selected
vector.
Rotate Elements will create one or more copies of the selected
elements, rotated around a selected point, at a specified angle per
copy. It is optional whether the original should be kept.
Scale Elements will create one or more copies of the selected
elements, scaled about a selected point by a specified scale factor. It
is optional whether the original should be kept.
Undo will undo one or more operations. This can mean deleting
elements created, restoring deleted elements, and/or undoing
modifications to elements. Undo can also be accessed with CtrlBackspace.
7.6. Milling
The Milling toolbar allows the user to perform various operations used in the manufacturing
of parts. All the operation can be exported directly to CIMCO Edit or to the clipboard, for
insertion in a user defined location. The functions in the Milling toolbar are also found under
Milling operations in the menu.
Face Milling creates a facing operation based on a selected outline
contour.
21
Pocket Milling creates pocket operations for one or multiple pockets.
These pockets can contain none or multiple islands. In a single
operation, it is possible to make both roughing and finishing cuts, but
only with one tool.
Contour Milling creates operations for contour milling. A contour
operation can machine multiple contours with roughing and finishing
cuts, but only with one tool.
Drilling creates drilling operations for hole drilling. From a drawing
the hole positions can be selected with the use of a filter, or by
simply indicating the hole position. If multiple holes are drilled, they
can be arranged in both rectangular and circular patterns.
Helix Milling can generate operations for helix drilling. Like normal
drilling, multiple holes can be selected with the use of filters, or by
selecting the individual circles on the drawing.
Thread Milling can create threading milling operations. The threads
can be inside or outside, and can be created for tools with one or
multiple teeth. Again multiple threads can easily be selected with the
use of the filter function.
Simple letter milling can generate operations for milling simple
letters on the drawing. These letters will have to be drawn using the
simple letter function, but then all letters can be selected with the
window functions, and machined in operations based on their start
and end depth.
True Type letter milling can create operations to mill the outline and/
or the interior of the individual letters. The letters can be selected
with the window function, and all letters with the same parameters
can be machined in one operation.
22
Export Contour can export a contour that the operator has selected
on the drawing. If a controller have smart canned cycles for example
a specific pocket operation, the user can create a macro in the editor
to support this, and then export the actual contour for insertion in the
canned cycle.
Feed and Speed Calculator is used to generate tool changes, or to
simply calculate the feed and speed, based on the data of a specific
tool.
23
8. Menus
Most of the CNC-Calc v2 functions are accessed through the CNC-Calc menu, however, the
following functions are accessed through the File menu.
8.1. File menu
CloseCloses the active file. If the active file has been modified, then the user will be prompted to save it. Close can also be accessed
with Ctrl-F4.
Close All Closes all open files. If any files have been modified, then the
user will be prompted to save them.
SaveSaves the drawing to your hard disk. If it is the first time you
save the drawing, you will be prompted for a file location and
name. Save can also be accessed with Ctrl S.
Save As Saves the drawing under a different name.
ExitCloses CIMCO Edit v5, and thus also CNC-Calc v2. If any
files have been modified, then the user will be prompted to
save them. Exit can also be accessed with Alt F4 (Alt F4 is a
Windows standard).
8.2. CNC-Calc menu
New Drawing Clears the graphics area (you will get a chance to save any
unsaved changes). New can also be accessed with Ctrl N.
Open Drawing Opens an existing CNC-Calc v2 file. Open can also be accessed
with Ctrl O.
24
8.2.1. Draw Points / Lines
Point Draws a point at the selected position
Between 2 points Draws a line between the two selected points.
Vertical Draws a vertical line. The first point selected defines the
starting point (and the X coordinate), the second point selected
defines the length (and need not be directly above or below the
first point).
Horizontal Draws a horizontal line. The first point selected defines the
starting point (and the Y coordinate), the second point selected
defines the length (and need not be directly to the left or right
of the first point).
Polar Lets you select the starting point of a line, and you then select
(or write) the angle and length of the line.
Perpendicular Draws a line perpendicular to another line. You first select the
line your new line is to be perpendicular to, then the starting
point of your new line. You then select the length of your new
line, and last you select in which direction from the starting
point your new line is to go.
Parallel Draws a line parallel to another line. You first select the line
your new line is to be parallel to, then the starting point of your
new line. You then select the length of your new line, and last
you select in which direction from the starting point your new
line is to go.
Bisector Draws a line bisecting two other lines, i.e. a line that halves the
angle between two lines. You first select the two line you want
to bisect, then you select the length of your new line (from the
intersection of the two lines you are bisecting), and last you
select which of the four possible solutions you want to keep.
Tangent Two Elements Lets you draw a line tangent to two circles or arcs. You select
the two circles or arcs your new line is to be tangent to, and
then you select which of the solutions you want to keep.
25
Tangent Angle Draws a line tangent to an arc or circle, at a selected angle. You
first select the arc or circle your new line is to be tangent to,
then the angle and length, and last you select which of the two
solutions you want to keep.
Tangent Through Point Draws a line tangent to an arc or circle, to a selected point. You
first select the arc or circle your new line is to be tangent to,
then the point it is to go though, and last you select which of
the two solutions you want to keep.
Rectangle Draws a rectangle where you select the two opposite corners.
It is possible to define a corner radius for the rectangle (the
corner radius is ignored if there is not room for it).
8.2.2. Draw Arcs / Circles
Two PointsLets you define the circle by selecting two (diametrically
opposite) points.
Three Points Lets you define the circle by selecting three points on the
periphery of the circle.
Center Radius Lets you define the center of the circle, followed by the radius.
Center Diameter Lets you define the center of the circle, followed by the
diameter.
Tangent Two ElementsLets you define a circle tangent to two elements, of a defined
radius. You first write the radius, then you select the two
elements the circle is to be tangent to. Last you select which of
the solutions you want to keep.
Tangent Three Elements Defines a circle tangent to three elements. You select the three
elements the circle is to be tangent to, and then you select
which of the solutions you want to keep.
Tangent Center on Line Lets you define a circle tangent to one element, with its center
on a line, of a defined radius. You first write the radius, then
26
you select the line the center is to be on, and the element the
circle is to be tangent to. Last you select which of the solutions
you want to keep.
Tangent through Point Lets you define a circle tangent to one element, through a point,
of a defined radius. You first select the point the circle is to go
through then write the radius, and select the element the circle
is to be tangent to. Last you select which of the solutions you
want to keep.
Two Points Lets you draw an arc by selecting the endpoints of the arc,
entering the radius, and selecting which solution you want to
keep.
Three Points Lets you draw an arc by selecting three points. Note, that the
arc created will not cross the zero degree point (3 o’clock); The
order the three points are selected in does not matter.
Start and End Angles Lets you define an arc by its center point, radius, starting angle
and end angle.
8.2.3. Draw Special
Rectangular Bolt Hole Pattern
Defines a rectangular bolt pattern. You select the start point
(one of the corners), and then enter the step in X, step in Y,
number of holes in X, number of holes in Y and the hole
diameter.
Circular Bolt Hole Pattern Defines a circular bolt pattern. You select the center of the bolt
pattern, select the radius of the bolt pattern, and then enter the
start angle, step angle, number of holes and the hole diameter.
Simple Text Linear Alignment
Defines simple text written on a line. You enter the start point,
angle of the line, then the distance between and height of the
27
letters. It is also possible to select the horizontal and vertical
alignment of the text.
Simple Text Circular Alignment
Defines simple text that is written on a circle. You select or
enter the center and radius of the alignment circle, then the
start angle, space between and height of the letters. It is also
possible to select the horizontal and vertical alignment of the
text, on the circle.
True Type Text Linear Alignment
Defines True Type text written on a line. You enter the start
point and angle of the line, and then the height of the letters. It
is also possible to select the horizontal and vertical alignment
of the text.
True Type Text Circular Alignment
Defines True Type text that is written on a circle. You select
or enter the center and radius of the alignment circle, then the
start angle and height of the letters. It is also possible to select
the horizontal and vertical alignment of the text, on the circle.
8.2.4. Modify
Trim To Intersection ill trim the selected element to the nearest intersection(s).
W
Select the element to be trimmed on that part to be removed; it
is then trimmed to the intersection(s) nearest the point where
it was selected. The trimmed element is also broken in two, if
there are intersections on both sides of the selected point.
Trim One Element Will trim one element to another. Select the element to be
trimmed first, on the side to be kept, and then select the
element to trim to.
28
Trim Two Elements ill trim two elements to each other. Select the two elements
W
to be trimmed, on the side to be kept.
Fillet Elements Creates a fillet between two elements, with a fillet radius the
user selects. It is optional, whether the two elements should
also be trimmed to the fillet.
Break Elements Will divide an element into two pieces. First select the element
to be broken into two, and then select the point at which it
should be divided.
Join Elements Will join two selected elements into one. The two elements
have to elements that can be joined into one element, of course.
Delete Will delete the elements you select. They can be restored with
the Undo function (the icon or Undo under Modify in the
menu.
Offset Will offset the elements you select by a specified distance. It is
optional whether the original should be kept.
Mirror Elements will mirror the elements you select about a line selected as the
mirror axis.
Translate Elements Will translate the elements you select along a vector defined by
selecting two points. It is optional whether the original should
be kept, and it is possible to create multiple copies, where each
copy is translated one step further along the selected vector.
Rotate Elements Will create one or more copies of the selected elements, rotated
around a selected point, at a specified angle per copy. It is
optional whether the original should be kept.
Scale Elements Will create one or more copies of the selected elements, scaled
about a selected point by a specified scale factor. It is optional
whether the original should be kept.
Undo Will undo one or more operations. This can mean deleting
elements created, restoring deleted elements, and/or undoing
modifications to elements. Undo can also be accessed with
29
Ctrl- Backspace.
Zoom in Centered on the middle of the graphics area. Zoom in can also
be accessed with Page Down.
Zoom out Centered on the middle of the graphics area. Zoom out can also
be accessed with Page Up.
Zoom All Will fit the drawing to the graphics area. This can also be done
by clicking the middle button on the mouse (on most mice,
pressing the scroll wheel), or with Ctrl-End.
Zoom Window Lets you zoom in on an area, which you select by first clicking
at one corner, then dragging the rectangle and clicking at the
opposite corner.
Snap to Grid Snaps to the grid points.
Snap to Points Snaps to points drawn by the user.
Snap to Center points Snaps to the centers of circles and arcs.
Snap to Mid points Snaps to the midpoints of elements.
Snap to End points Snaps to the endpoints of elements.
Snap to Intersections Snaps to the intersections between elements.
Enable All Snap Types Activates all snap types.
Disable All Snap Types Deactivates all snap types.
Layout Toolpath Lets you chain a toolpath contour, and then export it as ISO or
Heidenhain Conversational NC code.
Drill Holes Lets you select drill points and a drill cycle, and then export it
as ISO or Heidenhain Conversational NC code.
Setup CNC-Calc Lets you access the configuration for CNC-Calc.
30
8.2.5. Milling Operations
Face Milling Creates a facing operation based on a selected outline contour.
Pocket Milling Creates pocket operations for one or multiple pockets. These
pockets can contain none or multiple islands. In a single
operation, it is possible to make both roughing and finishing
cuts, but only with one tool.
Contour Milling Creates operations for contour milling. A contour operation can
machine multiple contours with roughing and finishing cuts,
but only with one tool.
Drill Holes Creates drilling operations for hole drilling. From the drawing
the hole positions can be selected with the use of a filter, or
by simply indicating the hole position. If multiple holes are
drilled, they can be arranged in both rectangular and circular
patterns.
Helix Drilling Generates operations for helix drilling. Like normal drilling,
multiple holes can be selected with the use of filters, or by
selecting the individual circles on the drawing.
Thread Milling Creates threading milling operations. The threads can be inside
or outside, and the can be created for tools with one or multiple
teeth. Again multiple threads can easily be selected with the
use of the filter function.
Mill LettersGenerates operations for milling simple letters on the drawing.
These letters will have to be drawn using the simple letter
function, but then all letters can be selected with the window
functions, and machined in operations based on their start and
end depth.
Mill True type Letterscreates operations to mill the outline and/or the interior of the
individual letters. The letters can be selected with the window
function, and all letters with the same parameters can be
machined in one operation.
31
Export Contour
Can export a contour that the operator has selected on the
drawing. If a controller has smart canned cycles for example
a specific pocket operation, the user can create a macro in the
editor to support this, and then export the actual contour for
insertion in the canned cycle.
CalculatorThe feed and speed calculator is used to generate tool changes,
or to simply calculate the feed and speed, based on the data for
a specific tool.
32
9. Configuring CNC-Calc
Perhaps the most important thing to remember when configuring CNC-Calc is that, except
for the toolbar positions, the configuration is specific to each machine type.
9.1. Main configuration
The main configuration is easiest to enter by selecting CNC-Calc → Setup CNC-Calc or
Setup → CNC-Calc from the menu, or the
icon from the CNC-Calc Tools toolbar. It can
also be entered by selecting Setup → Machine / File Types from the menu or the
icon
from the file operations toolbar, and then selecting CNC-Calc from the configuration tree.
It is important to select the correct machine type, and it should be noted, that the selection
between ISO and Heidenhain conversational NC code output is made by the template used
when creating the machine type. The window below shows the main configuration dialog.
33
It is important to select the correct machine type, and it should be noted, that the selection
between ISO and Heidenhain conversational NC code output is made by the template used
when creating the machine type. The window below shows the main configuration dialog.
The top part of the CNC-Calc configuration dialog contains the settings for toolpath output,
with the settings for the drawing grid at the bottom. The correct settings for toolpath output
depend on the machine and control that is to run the NC code. You should consult the
programming manual for your specific machine if in doubt.
The settings for toolpath output are:
Turning Select this for turning (lathe) output. This option is unavailable
for Heidenhain conversational NC code output.
Diameter programming (lathe)
Selects whether X axis output is in diameter measurement or
in radius measurement. This option is only available if turning
(lathe) output is selected.
Arc center is specified as diameter (lathe)
Selects whether the I value for arcs is specified in diameter
measurement or in radius measurement. This option is only
available if turning (lathe) output is selected.
Always add sign Selects whether to always output the sign of the coordinate
(giving a + sign on positive and zero coordinates), or whether
the sign is only output on negative coordinates.
Show plot as positive X/I (lathe)
Selects whether the X/I output is in the X+ or the X- direction.
This option is only available if turning (lathe) output is
selected.
Modal X/Y values Selects whether the coordinates are modal or not. Modal
coordinates means coordinates are only output when changed,
while non-modal coordinates means both X and Y are output
on every line, regardless of whether they are changed or not.
34
Show grid Select this to make the grid visible.
Machine Type Select the machine that the output should be formatted for. For
milling this could be Heidenhain or ISO milling.
Arc Type
Absolute arc center The arc center is given in absolute I and J
coordinates.
Relative to start The arc center is given in I and J coordinates, relative
to the start point of the arc.
Radius (R) values The arc radius is given (with the address R), rather
than the arc center.
Number of decimals All coordinates are rounded to this number of decimals, and if
padding with trailing zeroes is selected below, coordinates are
padded with trailing zeroes to this number of decimals.
Trailing 0’s
X123.000Coordinates are padded with trailing zeroes to the
number of decimal selected above, if rounding results
in fewer non-zero decimals.
X123.0 Whole numbers are output with one trailing zero.
Other coordinates are output rounded to the number
of decimals selected above, without trailing zeroes.
X123Whole numbers are output with a decimal point,
with no trailing zeroes. Other coordinates are output
rounded to the number of decimals selected above,
without trailing zeroes.
Maximum arc output angle This is primarily used in milling, and it allows the operator to
control the maximum sweep of the arcs. Some controllers can
not handle arcs with a sweep larger than 180 degrees, and here
it is possible to ensure that these arcs will not be generated.
35
Rotary axisIf Y-axis substitution is used, this field contains the address
letter of the axis used in this substitution.
Rotary axis linearization tolerance
When axis substitution is used all Y-axis movements are
transformed to an axis rotation. To control the precision of this
transformation, the entered linearization tolerance is used.
The grid settings are:
Grid size This sets the spacing between main grid points.
Show sub-gridSelect this to have a sub-grid visible when zoomed in to a
degree that shows few main grid points.
Show origin
Select this to have lines along X and Y zero visible.
36
10.Color configuration
The Color configuration is entered by selecting Global Colors in the configuration tree (after
entering the configuration and selecting the correct machine type), and scrolling down to the
CNC-Calc colors in the list.
To change the color of a CNC-Calc element, either left click the element in the list to select
it and click the select color button
, or you can double-click the element in the list. The
color can then be picked from a standard palette, or a custom color can be defined.
37
11.Other configurations that
affect CNC-Calc
There are a few other configurations in CIMCO Edit v5 that affect CNC-Calc.
Machine type template As has already been mentioned, the template used when
creating a machine type determines whether the NC code
output from CNC-Calc is in ISO or Heidehain conversational.
Machine under file types In the Machine dialog under File types in the configuration, the
Comment start, Comment end and Decimal point settings are
used by CNC-Calc when creating NC code.
38
12.Tutorial 1
2D Construction
This tutorial demonstrates one of many ways in which the 2-dimensional part above can be
drawn in CNC-Calc v2. Since the part consists of a number of similar elements and since
its part-elements are symmetrical, only a subsection of the part needs to be drawn. The
rest emerges from mirroring and finally joining the mirrored elements with straight lines
completes the part.
This tutorial demonstrates the use of the following functions:
•
•
•
•
•
•
•
•
•
Draw a rectangle with a corner radius
Draw a circle with known center and radius
Draw vertical and horizontal lines from known points
Offset a circle
Make curves between elements
Delete elements
Mirror elements about lines
Join end points with straight lines
Save file with name of your own choice
39
12.1. Before you start
The first thing to do before drawing a new part is to set the menu parameters. Start CIMCO
Edit v5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown in
the image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar
area.
To make a new drawing you must click on CNC-Calc and then select New Drawing.
40
The following window should now be displayed:
NoteIf you hold the cursor over an icon a short description of its functionality
will appear.
You can change the colors of the drawing area by selecting Setup and
then Colors from the dropdown menu.
41
12.1. Draw the geometry
Draw a rectangle with sides = 150, height = 100 and corner radius = 12.5
Click on
in the toolbar and enter the
following values:
First Corner X First Corner Y Second Corner X Second Corner Y Corner Radius Click on
= 75
= 50
= -75
= -50
= 12.5
to approve the command.
Draw a circle with radius = 5 defined by its center
Click on
in the toolbar.
Enter Circle Radius = 5
Activate the snap function
(circles center points).
Snap to the center of the left topmost
corner arc.
Left-click to add the circle.
42
Draw a vertical and horizontal line defined by its end point and length
Activate the snap function
(circles center
points) and
(midpoint of lines).
Click on
and enter the following into the
dialog: (-20.0000).
Snap to the center of the left topmost corner
arc.
Click to add the vertical line.
Snap to the midpoint of the topmost horizontal
line.
Click to add a vertical line. This will serve as a
mirror line for the mirroring of our part about
the Y-axis.
Similar to the above draw a horizontal line with length = 20 from the same center. This time
Line Length is set to 20 and next the mirror line is added from the center of the left horizontal
line (the X-axis, see picture below).
43
Offset a circle
Click on
in the toolbar and enter:
Offset Distance = 7.5 (12.5 - 5 = 7.5).
Click on the circle and select the outermost of the appearing circles.
Your drawing should now look like the one below.
44
Create a fillet between elements
Click on
in the toolbar.
Enter Fillet Radius = 5.
B
A
Click on the circle by A and on the line by B.
From the possible solutions select the part of the circle, which makes the right fillet. In the
picture below you can see how it should look.
Do the same by the vertical line.
The topmost left part of your drawing should now
look similar to the picture on the right.
Click on
and delete the two lines by C (The ones
pointing out from the center of the circle).
C
45
Mirror elements about mirror lines
Click on
in the toolbar.
First, click on the vertical mirror line.
Click on all the elements, which should be mirrored (the circle and the inner corner). You can
hold down the left mouse button while dragging out a window around the elements.
Now do the same and mirror about the horizontal mirror line. Continue mirroring until your
drawing looks similar to the one below.
Click on
and delete the mirror lines.
46
Connect the inner elements
Activate this snap function
Click on
(snap to end points).
in the toolbar.
Snap to the two arcs end points and add the remaining horizontal and vertical lines to finish
the part.
Your part should now look as the one below.
Name the file and save it
Click on Files and then select Save as from the dropdown menu. Give the file a new name
and save it (the file extension is added automatically).
47
48
13.Tutorial 2
CNC-toolpaths and Face milling
With CNC-Calc v2 it is possible to create toolpaths directly from the program’s geometrical
drawings. Thereby calculations become more secure and programming becomes much
faster compared to doing it manually. At the same time you get a big advantage since it is
possible to move, copy, rotate, scale and mirror elements with the result of instant NC-code
generation.
This tutorial demonstrates how the 2-dimensional part above can form the basis for NC-codes
for various types of machining.
Note
This tutorial builds upon the result from CNC-Calc v2 Tutorial 1.
49
13.1. Before you start
The first to do before drawing a new part is to set the menu parameters. Start CIMCO Edit
v5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown in the
image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar area.
To make a new drawing you must click on
CNC-Calc and then select New Drawing.
Alternatively the same can be achieved by
clicking on the folder icon
in the toolbar.
Select the file from CNC-Calc Tutorial 1 and
click open.
50
You should now see the part from CNC-Calc v2 Tutorial 1 displayed in front of you.
NoteIf you hold the cursor over an icon, for a moment, a short description of
its functionality will appear.
51
13.1. Creation of Facing toolpaths
To begin with select what format the NCprogram should be programmed in by arrow A.
A
Select: ISO Milling.
Then select Generate a CNC-Toolpath for
Face Milling by clicking on the icon by arrow
B.
Write the text FACING in the Comment field.
This text will be present at the start of the final
NC code for this operation. When multiple
operations exist in the same NC program, it
will help to locate and identify the start of each
operation.
Click on the outlining contour at the place
indicated by arrow C.
This will select the bounding contour that the
facing operation will operate on.
Click on Parameters by arrow D.
Enter the following values into the dialog
shown to the right.
Cutter Diameter:
This is the diameter of the cutter. Here it is a 30
mm Face Mill.
Start Depth: This is the top of the part.
End Depth: The final depth (will be corrected
by Stock to Leave).
B
C
D
52
Retract Height: When the operation is
finished, this is the height that the tool will
retract to. Roughing Stepdown: This is the
maximum roughing cuts that the operation will
take.
Finish Stepdown: If Finish Cuts larger than
zero, this is the cut that will be taken in each
finish cut.
Finish Cuts: This is the number of finish cuts
that the operation will perform. If the value is
left at zero, only roughing cuts will be made.
Enter the following values into the dialog,
which is shown to the Right.
Cutting Method: This is the method used to
perform the face operation. It is possible to
select Zigzag, Climb or Conventional.
Move Between Cuts: This is only used for
the Zigzag Cutting Method, since the other
methods will move free between cuts.
Overlap Across: This is the amount that the
mill will hang out over the side diagonal to the
cutting direction.
Overlap Along: This is the distance that the
tool will move out over the end before the high
speed loops are taken.
Entry Distance: Is the distance that the tool
will start out at before the actual cut is taken.
Exit Distance: This is the distance the tool
moves out after the final cut is taken.
53
Facing Angle: Is the angle that the operation
is performed at. An angle of zero is along the
X-axis, and an angle of 90 is along the Y-axis.
Now close the parameters dialog with OK and click on Export Editor. The following screen
should now be displayed.
13.2. Inserting a Tool with Feed and Speed Calculator
The Feed and Speed calculator is build into CNC-Calc, and it is used to insert feed and speed
data into the NC program. All the data used in the calculations can normally be found in the
reference material supplied by the manufacturer.
In the facing example, we used a face mill that we give the following characteristics:
diameter is 30mm, it has 5 flutes, a cutting feed of 0.08mm per tooth and a cutting speed of
190mm/min.
54
In order to use the feed and speed calculator,
select Feed and Speed Calculator for
Milling Operations by clicking on the icon
indicated by arrow A.
A
Fill in the following values:
Tool # lets say that the face mill have a
tool number of 1.
Diameter was 30mm.
# Flutes: The number of flutes was 5.
Feed per tooth:
In this example it is set to 0.08mm
Cutting Speed: Is set to 190.
The fields are linked together, so as soon as
entries are made in the cutting speed field,
the other fields will be updated.
If we wanted to have RPM 2000 and a
feedrate of 800 instead of the calculated
2015 and 836.385, the value for the cutting
speed would be updated to 188.5.
Change the RPM to 2000 and the feedrate
to 800.
Click on Export Clipboard indicated by
arrow B.
B
55
The line for the NC program is now in the clipboard, and it is ready for insertion. Change the
window to the NC program, and move to the very start, by pressing Ctrl-Home.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit → Paste from
the drop down menu.
The NC program should now look similar to the one below.
Now save the NC program as CNC-Calc v2 Tutorial 2.NC
56
57
14. T
utorial 3
Contour milling
CNC-Calc v2 can generate contour milling - with and without radius compensation. There
are several machine types in CNC-Calc, but the most comonly used are ISO G-code
programming and Heidenhain plain text.
This tutorial demonstrates how the above 2-dimensional part can form the basis of NC-codes
for various types of machining.
Note
This tutorial builds upon the result from CNC-Calc v2 Tutorial 1.
58
14.1.Before you start
The first to do before drawing a new part is to set the menu parameters. Start CIMCO Edit
v5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown in the
image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar area.
To make a new drawing you must click on
CNC-Calc and then select New Drawing.
Alternatively the same can be achieved by
clicking on the folder icon
in the toolbar.
Select the file from CNC-Calc Tutorial 1 and
click open.
59
You should now see the part from CNC-Calc v2 Tutorial 1 displayed in front of you.
NoteIf you hold the cursor over an icon, for a moment, a short description of
its functionality will appear.
60
14.1.Creation of Contour toolpaths
In order to begin the creation of a NC program
for the contour operation select the Generate
CNC-Toolpath for Contour Milling by
clicking on the icon indicated by arrow A.
Write CONTOUR in the Comment field.
This text will be present at the start of the
final NC program. When multiple operations
exist in the same NC, it will help to locate and
identify the start of each operation.
Click on the outlining contour at the place
indicated by arrow B.
This highlights the outline contour, and the
direction of the arrows indicate the way the
tool will travel.
What side the tool will machine, is controlled
by the Work Side drop down box on the
General tab in the parameters dialog.
Click on Parameters by arrow C.
Enter the values in the dialogs as shown.
A
B
C
61
This dialog contains all the general parameters
that are used for roughing and finish in both
depth and side cuts.
Cutter Diameter:
Diameter of the tool in use.
Retract Height: The height where the tool
will move between contours, and where it it
will top at the end of the operation.
Safe Distance: This is the distance above
the part, where the feedrate will change from
rapid to cutting speed.
Start Depth: This is top of the stock.
End Depth: This is the depth where the last
cut will be taken. This value is corrected by
the Stock to leave Z value.
Stock to Leave XY: This is the amount of
stock that is left in the XY/side direction at
the end of the operation (after both Roughing
and Finish).
Stock to leave Z: The amount of stock that is
left in the Z/depth direction at the end of the
operation (after both Roughing and Finish).
Apply on Roughing Sidecuts: If this check
box is checked, the compensation type will be
applied to both roughing and finish side cuts.
Otherwise computer compensation is used for
roughing cuts, and the selected compensation
type for finish cuts.
Compensation Type: This is the
compensation type used for the operation.
62
Work Side: This field determines which side of the contour the tool will pass on. Together
with the selected direction of the contour, it determines if the milling type will be climb or
conventional.
Side cuts are the cuts taken in the XY direction.
Use Side Cuts: If this check box is checked
the operation will perform the cuts defined by
the parameters. Otherwise only one cut at the
final contour will be performed.
Number of Passes (Roughing): This is the
number of roughing side cuts in the operation.
Spacing (Roughing): If more than one
roughing pass is taken, this is the distance
between them.
Number of Passes (Finish): This is the
number of finish side cuts in the operation.
Spacing (Finish): This is the distance of each
finish pass.
Final Depth: If this check box is checked,
the finish passes will only be taken at the final
depth.
All Depths: If this check box is checked, the
finish passes will be taken at every depth.
Overlap Distance: This is the distance that
all the finish laps will overlap, in order to
smooth the surface.
63
Depth cuts are the cuts taken in the Z direction.
Use Depth Cuts: If this check box is checked
the operation will perform the cuts defined by
the parameters. Otherwise only one cut at the
final depth will be performed.
Max Roughing Steps: This is the maximum
cut that will be taken in a roughing cut.
Use Even Depth Cuts: If this check box is
checked, all the roughing passes will have the
same distance. If it is left unchecked, cuts will
be taken at the Max Roughing Steps distance,
and any rest material will be taken with the
last cut.
Number of Cuts (Finish): This is the number
of finish depth cuts in the operation.
Steps (Finish): This is the distance of each
finish pass.
Linearize Helix Movements: Some
machines can not make helix movements,
and if this check box is checked, all helix
movements will be converted to lines in the
NC operation.
Linearization Tolerance: When the helix is
converted to lines, this will be the maximum
error for the final lines.
By Depth: This is only used if multiple
contours are milled in the same operation.
If it is selected the cut on each depth will be
performed on all contours, before any cuts are
made at a new depth.
64
By Contour: If is selected one contour will be
milled from start to finish, before the next
contour is worked upon.
Lead in/out parameters describe the way the
tool will approach the contour at the start/end
of the roughing, and for each finish pass.
The use of lead in/out is optional when the
compensation is set to computer or none. It is
however mandatory, when any compensation
is performed by the controller.
Use Lead In/Out Parameters:
Enables or disables the lead in and out.
Use Line:
Enable or disables the lead in/out lines.
Line Length:
Is the length of the lead in/out line.
Perpendicular: If it is selected the line will
be perpendicular to the following element for
lead in, and the previous element for lead out.
Parallel: If it is selected the line will be
parallel to the following element for lead in,
and the previous element for lead out.
Use Arc:
Enables/disables the lead in/out arcs.
Radius: The radius of the lead in/out arc.
Sweep: Sweep angle of the lead in/out arc.
The two arrows in the middle of the dialog
are used to copy all values from lead in to out,
and the other way.
65
Now close the parameters dialog with OK and click on Export Clipboard. The NC
operation is now in the clipboard, and it is ready for insertion.
Change the window to the NC program, and move to the very end, by pressing Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit → Paste from
the drop down menu.
The NC program in the Editor now consists of two operations and currently they are both
made with the same tool. Now we need to insert a new tool for the contour operatio
14.2.Inserting a Tool with Feed and Speed Calculator
Follow the steps from the previous tutorial for the Feed and Speed. Instead of the values used
there, use the following values:
Tool #
Diameter (D) in mm
# Flutes (Z)
Feed per tooth (Sz) in mm
Cutting Speed (V) in mm/min
:2
: 10
:4
: 0.06
: 175
Now the last two values have been calculated and
inserted in the dialog. They should be:
RPM
Feedrate (F) in mm/min
: 5570
: 1336.9015
Correct the RPM to 5500 and then
Feedrate (F) in mm/min: to 1320.
Now the Feed and Speed dialog should look like the
one to the right:
66
Click on Export Clipboard to copy the generated line to the clipboard.
Change to the NC program in the editor. After the contour operation was copied to the editor,
the cursor is at the very end of the program. In order to insert the tool line from the clipboard,
we must locate the start of the contour operation. Since the comment CONTOUR was
inserted, it is easy to locate the start of the operation.
Find the text CONTOUR, either by pressing Ctrl-f, or selecting Edit → Find from the drop
down menu.
Go to the start of the comment line and insert the text from the clipboard. The NC program
should now look like the following.
Save the NC program as CNC-Calc v2 Tutorial 3.NC
67
15. T
utorial 4
Pocket milling
CNC-Calc v2 can generate pocket milling. There are several machine types in CNC-Calc, but
the most commonly used are ISO G-code programming and Heidenhain plain text.
This tutorial demonstrates how the above 2-dimensional part can form the basis of NC-codes
for various types of machining.
Note
This tutorial builds upon the result from CNC-Calc v2 Tutorial 1.
68
15.1.Before you start
The first to do before drawing a new part is to set the menu parameters. Start CIMCO Edit
v5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown in the
image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar area.
To make a new drawing you must click on
CNC-Calc and then select New Drawing.
Alternatively the same can be achieved by
clicking on the folder icon
in the toolbar.
Select the file from CNC-Calc Tutorial 1 and
click open.
69
You should now see the part from CNC-Calc v2 Tutorial 1 displayed in front of you.
NoteIf you hold the cursor over an icon, for a moment, a short description of
its functionality will appear.
70
15.1.Creation of Pocket toolpaths
In order to begin the create a NC program for
the pocket operation select the Generate a
CNC-Toolpath for Pocket Milling by
clicking on the icon indicated by arrow A.
Write the text POCKET in the Comment
field.
This text will be present at the start of the
final NC program. When multiple operations
exist in the same NC, it will help to locate and
identify the start of each operation.
Click on the inner contour at the place
indicated by arrow B. This will highlight the
inner contour.
Click on Parameters by arrow C.
This dialog contains all the general parameters
that are used for roughing and finish in both
depth and side cuts.
Enter the values in the various dialogs as
shown.
Cutting Diameter:
The diameter of the used tool.
Retract Height: The height where the tool
will move between contours, and where it it
will stop at the end of the operation.
Safe Distance: This is the distance above
the part, where the feedrate will change from
A
C
B
71
rapid to cutting speed.
Start Depth: This is top of the stock.
End Depth: This is the depth where the last
cut will be taken. This value is corrected by
the Stock to leave Z value.
Stock to Leave XY: This is the amount of
stock that is left in the XY/side direction at
the end of the operation (after both Roughing
and Finish).
Stock to leave Z: This is the amount of stock
that is left in the Z/depth direction at the end
of the operation (after both Roughing and
Finish).
Compensation Type: This is compensation
type used for the operation.
Conventional: When checked, the operation
will be generated using conventional milling.
Climb: When checked, the operation will be
generated using climb milling.
72
Side cuts are the cuts taken in the XY direction.
Use Side Cuts: If this check box is checked
the operation will perform the cuts defined by
the parameters. Otherwise only one cut at the
final contour will be performed.
Max Roughing Spacing: This is the
maximum side step over used in the roughing
of the part.
Number of Passes (Finish): This is the
number of finish side cuts in the operation.
Spacing (Finish): This is the distance of each
finish pass.
At Final Depth: If this check box is checked,
the finish passes will only be taken at the final
depth.
At All Depths: If this check box is checked,
the finish passes will be taken at every depth.
Overlap Distance: This is the distance that
all the finish laps will overlap, in order to
smooth the surface.
Roughing Smoothing: This slider controls
the amount of smoothing used. The higher the
value (rightmost), the smoother the resulting
toolpath will be.
73
Depth cuts are the cuts taken in the Z direction.
Use Depth Cuts: If this check box is checked
the operation will perform the cuts defined by
the parameters. Otherwise only one cut at the
final depth will be performed.
Max Roughing Steps: This is the maximum
cut that will be taken in a roughing cut.
Use Even Depth Cuts: If this check box is
checked, all the roughing passes will have the
same distance. If it is left unchecked, cuts will
be taken at the Max Roughing Steps distance,
and any rest material will be taken with the
last cut.
Number of Cuts (Finish): This is the number
of finish depth cuts in the operation.
Steps (Finish): This is the distance of each
finish pass.
Linierize Helix Movements: Some machines
can not make helix movements, and if this
check box is checked, all helix movements
will be converted to lines in the NC operation.
Linearization Tolerance: When the helix is
converted to lines, this will be the maximum
error for the final lines.
By Depth: This is only used if multiple
pockets are milled in the same operation.
If it is selected the cut at each depth will be
performed on all pockets, before any cuts are
made at a new depth.
74
By Pocket: If this is selected one pocket will be
milled from start to finish, before the next
pocket is worked upon.
The Entry Strategies define how the tool cuts
from one Z level to the next.
Plunge: When this is selected, the tool will
move straight down.
Ramp: With the ramp entry the tool moves
down to the Ramp Clearance above the part.
Then it makes a ramp movement with the
length Ramp Length and the angle Ramp
Angle.
Helix Entry: Moves down to Helix Clearance
above the part. Then it will spiral down with
the angle Helix Angle in a circular movement
with a radius between Helix Diameter and
Minimum Helix Diameter.
How big the actual diameter will be depends
on the geometry,
Lead in/out parameters describe the way that
the tool will approach the contour at the start/
end of the roughing, and for each finish pass.
The use of lead in/out is optional when the
compensation is set to computer or none. It is
however mandatory, when any compensation
is performed by the controller.
Use Lead In/Out Parameters: Enables or
disables the lead in and out.
Use Line: Enable or disables the lead in/out
lines.
75
Line Length:
Is the length of the lead in/out line.
Perpendicular: If it is selected the line will
be perpendicular to the following element for
lead in, and the previous element for lead out.
Parallel: If it is selected the line will be
parallel to the following element for lead in,
and the previous element for lead out.
Use Arc:
Enable or disables the lead in/out arcs.
Radius: Is the radius of the lead in/out arc.
Sweep:
Is the sweep angle of the lead in/out arc.
The two arrows in the middle of the dialog
are used to copy all values from lead in to out,
and the other way.
76
Now close the parameters dialog with OK and click on Export Clipboard. The NC
operation is now in the clipboard, and is ready for insertion.
Change the window to the NC program, and move to the very end, by pressing Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit  Paste from the
drop down menu.
The NC program in the Editor now consists of three operations, and since we use the same
tool for the contour and pocket operation we will not insert a tool in front of the pocket
operation.
Now save the program the NC program as CNC-Calc v2 Tutorial 4.NC
77
16. T
utorial 5
Backplot in the Editor
One of the advantages of running CNC-Calc inside CIMCO Edit v5 is that the editor can be
used to manipulate and backplot the NC programs generated in CNC-Calc. In the following
we will setup the backplot, and verify the program.
16.1.Before you start
The first thing to do before drawing a new part is to set the menu parameters. Start CIMCO
Edit v5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown in
the image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar
area.
78
To open a NC Program click the open
program icon.
This will open the Open File dialog, where
the file you want to open can be selected.
Please select the file from the last tutorial and
click open.
You should now see the NC program from the last tutorial.
79
16.2.The first backplot
When you have the NC program loaded in
the editor, it is possible to backplot it.
Click on the backplot icon in the floating
toolbar indicated by arrow A. This will open
the backplot window.
This window can also be opened by
Backplot → Backplot Window in the
dropdown menues.
A
Now the screen should look like the one below.
Here the toolpath is shown. It looks OK, but it can be configured to look a lot more like the
final part. To do this we need to define the individual tools, and the stock.
80
16.3.Backplot tool setup
The following steps will show you how to
setup the tools used in the backplot.
Click on the Tool Setup icon in the floating
toolbar indicated by arrow A. This will
open the backplot Tool definition window.
When backplot persed the NC program, it
detected, that there where two tools used.
Since these tools have not been defined, the
screen will look like the one to the left.
In order to backplot the program correctly,
we need to define these two tools.
By changing the type and the diameter of
the tools, we can create the correct setup.
Please select and enter the values shown on
the picture on the right.
These are the same tool values that was used
when the NC programs was generated in
CNC-Calc.
Now exit the configuration dialog with OK.
A
81
After the tools have been configured, the screen should look like the one below. Try to
find the tool changes and verify that the tool does endeed change when a tool change is
encountered in the NC program.
16.4.Backplot Stock setup
The following steps will show you how to
setup the stock used in the backplot.
Click on the Solid Setup icon in the floating
toolbar indicated by arrow A. This will open
the backplot Solid Setup window.
A
82
The default values shown in the dialog are
based on the cutting moves in the NC
program.
Since the tool moves down in cutting speed,
the Z-max will nearly always be too big.
The same is the case for the facing operation.
That will give a too large stock along both
the X- and Y- axis.
From the facing operation we know that the
top of the stock should be Z:2.00.
From the drawing we know that the values
of the corners are (0.00, 0.00) and (150.00,
100.00).
We now make the stock 2mm larger along
X- and Y-axis, so the values will be the ones
shown in the dialog on the right.
Please enter these and exit the dialog with
OK.
83
Now everything has been configured, and the backplot can now be used to verify the
operations. The screen should now look like the one shown below.
84
17. T
utorial 6
Drilling
CNC-Calc v2 can generate codes for drilling in either canned cycles or as longhand. There
are several machine types in CNC-Calc, but the most commonly used are ISO G-code
programming and Heidenhain plain text. Before you start
17.1.Before you start
The first to do before drawing a new part is to set the menu parameters. Start CIMCO Edit
v5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown in the
image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar area.
85
To make a new drawing you must click on
CNC-Calc and then select New Drawing.
Alternatively the same can be achieved by
clicking on the folder icon
in the toolbar.
Select the file from CNC-Calc Tutorial 1 and
click open.
You should now see the part from CNC-Calc v2 Tutorial 1 displayed in front of you.
NoteIf you hold the cursor over an icon, for a moment, a short description of
its functionality will appear.
86
17.2.Generate a drill cycle
To begin with select what format the
NC-program should be programmed in by
arrow A.
Select: ISO - Mill.
Then select Generate a drill Cycle by
clicking on the icon by arrow B.
Fill in the following values:
Name:
DRILL
Machine Zero X: 0
Machine Zero Y: 0
A
B
Click on Drill Parameters, which displays the window shown below.
Please enter these parameters for this drilling operation. Notice that in this example it makes
no Difference if we have selected Incremental or Absolute Safe Distance and Depth, since
these incremental values refer to the Reference Plane, which is 0.
87
For the selection of the location of the holes several options are available:
1. S
elect each hole location with the cursor. In order to get the correct hole center
for circles and arcs, the snap to center should be used
2. S
elect the actual circle or arc. This will create a new hole location, at the center
of the circle/arc.
3. U
se window selection with or without filter. If the filter is used it is possible to
limit the selection to cirles or arcs in different ranges.
4. I n the following we will use the filter to select the corner holes, but not any of the
arcs.
In the following we will use the filter to select the corner holes, but not any of the arcs.
By setting up the filter as shown, we will
limit the window selection to include only
circles in the range from 0 to 10 in diameter.
Now enable the Use Selection Filter in the lefthand pane, and then make a window selection,
that includes the entire drawing. When this selection is made, only the four corner holes
should be selected.
88
Click on Export Editor. The following program is displayed in the editor.
(DRILL)
G00 X12.5 Y87.5
G00 Z10.0
G83 X12.5 Y87.5 Z-7.0 R2.0 Q1.0 F200.0
X137.5
Y12.5
X12.5
G80
The order of operation can then be changed by clicking on Reorder Circ and Reorder Rect
in the dialog.
89
18. T
utorial 7
Milling of Letters
This tutorial demonstrates how a 2-dimensional text can be used as the basis for an NC
program milling letters and numbers.
18.1.Before you start
When a new part is to be machined you should first make sure to display the toolbars you
need. Start CIMCO Edit 5, click the dropdown menu Setup, and then click Show Toolbars.
Now select the needed toolbars as shown below. Clicking an already selected toolbar in the
list deselects it.
Notice This menu can also be reached by right-clicking any toolbar already in view.
90
Once the toolbars have been selected you are
ready to start on a new drawing.
To do this click on the icon
or click on
CNC-Calc in the menu, and then on New
Drawing.
In this tutorial we will try to machine a single
line of text composed of letters and numbers.
For this example we have chosen the text
“CIMCO 123”.
Normal upper and lower case letters,
numbers, and characters can be entered when
the icon
is clicked.
The dialog Text Entry appears to the left. In the input field at the bottom named text, enter
the text that will be machined. In this example “CIMCO 123”.
In addition to the text five additional parameters are needed to specify start point, baseline
angle, letter distance and letter height. Fill in the fields with the values from below.
X coordinates of the text start point:
Y coordinates of the text start point:
Angle of the text baseline:
Distance between letters:
Letter height:
-68 -30 15 6
25 (mm)
(mm)
(deg.)
(mm)
(mm)
When you are done entering text and values click the blue check mark button
bottom right of the dialog to accept.
at the
91
Your screen should now look like the following.
The text is now showing in the drawing and its geometry can now be used for generating the
toolpaths.
Select the file type (NC Format) for our
example letter milling program (e.g. ISO
Milling).
92
Select the feature Letter Milling by clicking the CNC-Calc menu, then Millng Operations,
Mill Letters, or select the corresponding icon
from the Milling Operations toolbar.
The dialog Letter Milling will appear on the left side of the screen as shown above.
Further, you should also click on the Parameters button to
define e.g. retract height over the part surface. For this
example we chose a 2 mm. retract height, see on the right.
Besides Retract Height you can choose if retracts should be
carried out in rapid or feed mode. Once finished click OK
to close the Parameters dialog..
93
Now use window selection to select the text you want to mill. On the drawing left-click one
corner, hold down the mouse button and drag diagonally. When the desired text is framed,
release the button. The frame disappears and the text will have turned yellow to indicate that
it has been selected.
Next click on the Export Editor button, and this will show the NC codes for machining the
text in the Editor.
To verify the generated toolpath we must
simulate it using the integrated Graphical
Backplot. To open the backplot window click
on Backplot in the menu and then on
Backplot Window as shown below.
At the bottom right of the backplot window,
start the simulation by clicking Start/Stop
Simulation indicated by the icon
.
Simulation speed and direction is infinitely
variable both forwards and backwards. This is
controlled by dragging the slider either to the
left or to the right where right is forward.
94
If you want to verify a certain operation in the NC program, simply click on a line of the NC
code to the left. The simulation tool will immediately position itself on the corresponding
place in the simulation. You can move the tool one line at a time using the up and down
arrow keys on your keyboard, or skip through the code a page at a time using PageUp and
PageDown.
Your screen should now present “CIMCO 123” in the following way.
Notice the rapid moves, indicated by the yellow lines, retracting to the level we defined using
the Parameters dialog.
The example text milling program “CIMCO 123” can be used as subprogram to another
program by simple cut-and-paste, but can also be completed as an independent program,
providing it is supplied with the code lines for Program Start/Program Stop, Tool Change,
and Feed/Speed, which you can quickly add either manually or with the Macro function in
CIMCO Edit 5.
Important notice
The final execution of the program depends to a high degree of the applied macro programs.
It is also important that the correct set-up of CNC-Calc is used for each machine/control.
95
It is very important to verify/simulate the programs before they are executed on a
machine. Please pay special attention to the movements in the Z axis, and make sure
that they run with the required feed and rapid move speed.
96
19. T
utorial 8
Milling of TrueType Letters
This tutorial demonstrates how a 2-dimensional TrueType text can provide the basis for an
NC program milling letters and numbers.
19.1.Before you start
When a new part is to be machined you should first make sure to display the toolbars you
need. Start CIMCO Edit 5, click the dropdown menu Setup, and then click Show Toolbars.
Now select the needed toolbars as shown below. Clicking on an already selected toolbar in
the list deselects it.
Notice This menu can also be reached by right-clicking
any toolbar already in view.
97
To start a new drawing, either click on the icon or click on CNC-Calc in the menu, and then
on New Drawing.
In this tutorial we will machine a single line of TrueType text composed of letters and
numbers. For this example we have chose the text “CIMCO 456”.
To create TrueType letters, numbers, and characters select the function Create TrueType
text in drawing by clicking on
.
The dialog Text Entry appears to the left. Enter the coordinates for the starting point of
the text, the angle (relative to the horizontal axis) of the text baseline, and the height of the
letters.
X coordinates of the text start point:
Y coordinates of the text start point:
Angle of the text baseline:
Letter height:
-68
-30
30,0
25,0
(mm)
(mm)
(deg.)
(mm)
In the bottom field you write the text (here “CIMCO 456”) to be milled with TrueType
letters.
98
Next select the font type and font size by opening the font dialog by clicking on the button
Select Font. End this dialog by clicking ‘OK’. As a result of the changes you make in the
font dialog the look of the text changes. You can enter the font dialog again until you are
satisfied with the layout.
When done click on the blue check mark button
to insert the text. This is important since
otherwise the text will disappear once you start doing other things.
99
With parameters, text, and font defined your screen should look like the following.
Depending on your choice of font this might vary.
The geometry is now finished and can be used for the generation of toolpaths.
Now select the file type (NC format) for the
TrueType text mill program (e.g. ISO
Milling).
100
From the CNC-Calc menu, select Milling Operations and Mill TrueType letters, or click the
corresponding icon
on the toolbar.
The Letter Milling dialog has now appeared to the left. Click on the Parameters button.
The TrueType Text Milling Parameters dialog appears. Check the Mill Outline checkbox
at the top and fill in the rest of the fields as shown below. Click ‘OK’ when done.
101
Use window selection to select the letters to mill. This is done by left-clicking in the upperleft corner of the drawing. Now hold the mouse button down and drag the cursor to the
lower-right corner and release the mouse button. Click on the button Show Toolpath. Now
the screen will show the generated toolpaths which is layed out directly over the outline of
the text (it might be hard to see). Finally click on the button Export Editor.
Now the NC-codes for the machining are shown in the editor. Use the Graphical Backplot to
simulate and verify the toolpaths. To start the backplot click on the Backplot menu and then
on Backplot Window.
Use the buttons in the lower-right corner of the window to control the simulation speed and
direction. By clicking on a line in the NC-code to the left the tool will jump to that position
in the simulation. The up and down key moves the line selection to the previous or next line,
and the tool will be moved acordingly.
102
19.2.Pocket milling letters
The toolpath generated from the text look like a contour operation formed by the outlines of
the letters and numbers. The area inside these contours - inside the letters - can be milled like
a special pocket milling operation. The rest of this tutorial will show you how to do this.
1. Return to the drawing by clicking the tab marked A in below image.
1. Click on the button New marked B, and select the letters for the operation.
1. Click the button Parameters marked C.
1. I nsert the new parameters as shown below (remember to check the 5. checkbox
Mill Interior).
D
B
A
C
103
1. Window select the text.
1. C
lick on Show Toolpath marked D - the generated toolpaths will now be shown
on the screen.
1. C
lick the button Export Editor. Now the NC-codes for the machining are shown
in the editor
104
Simulate the program to verify the toolpath the same way we did earlier in this tutorial.
It is possible to generate toolpaths with both Mill Interior and Mill Outline selected under
Parameters. This will create both the pocket operation on the inside, and the milling of the
contours.
The example program “CIMCO 456” can be used as subprogram to another program by
simple cut-and-paste, but can also be completed as an independent program, providing it is
supplied with the code lines for Program Start/Program Stop, Tool Change, and Feed/Speed,
which you can quickly add either manually or with the Macro function in CIMCO Edit 5.
Important notice
The final execution of the program depends to a high degree of the applied macro programs.
It is also important that the correct set-up of CNC-Calc is used for each machine/control.
It is very important to verify/simulate the programs before they are executed on a
machine. Please pay special attention to the movements in the Z axis, and make sure
that they run with the required feed and rapid move speed.
105
20. T
utorial 9
Drawing the part
2D construction of a part for turning
This example demonstrates one of many ways in which the 2-dimensional part above can
be drawn in CNC-Calc v2. Since the part consists of a number of similar elements and
since its part-elements are symmetrical only a subsection of the part needs to be drawn. The
rest emerges from mirroring and finally joining the mirrored elements with straight lines
completes the part.
This tutorial demonstrates the use of the following functions:
•
•
•
•
•
•
•
•
•
Draw a vertical line defined by its starting point and length.
Offset a geometric element.
Draw a circle with a given radius defined by its centre.
Draw a line defined by its end points.
Draw a horizontal line defined by its start point and length.
Draw a line defined by its start point, angle, and length.
Trim element between points of intersection with other elements.
Connect and round with a given radius between two elements.
Connect and bevel two elements by a given angle and distance.
106
20.1.Before you start
The first thing to do before drawing a new part is to set the menu parameters. Start CIMCO
Edit v 5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown
in the image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar
area.
To make a new drawing you must click on
CNC-Calc and then select New Drawing.
107
The following screen should now be displayed.
Note
If you hold the cursor over an icon a short description of its functionality will appear.
You can change the colors of the drawing area by selecting Setup and then Colors from the dropdown menu. For this tutorial we have chosen to use red as our drawing color and white for the background.
108
20.2.Draw the geometry
Draw vertical lines defined by start point and length
Click on
values:
in the toolbar and enter the following
Start Point of Line Z = 0
Start Point of Line X = 0
Line Length = 12
Click on
to approve the command.
If the axis are shown it can be difficult to see the line
since it is on the X-axis
Draw another vertical lines defined by start point and length
Enter the following values in the dialog that is already
open:
Start Point of Line Z = -110
Start Point of Line X = 0
Line Length = 25
Click on
to approve the command.
Click on
in the zoom toolbar. This will make the drawing fill the whole drawing area on
the screen.
109
Offset an element
Click on
values:
in the toolbar and enter the following
Offset Distance = 80
New click on the leftmost line indicated by A on the
picture below.
After this is done two lines will appear (only the
rightmost can be seen on the drawing). Now click to
the right of the selected line to keep the line shown
in red.
A
110
Draw a circle with radius = 25 defined by its center
Click on
in the toolbar.
Center Point Z = -110+50 (-60)
Center Point X = 70
Enter Circle Radius = 25
Click on
to approve the command.
Draw a line defined by its endpoints.
First click on
below.
to activate the snap function ‘Snap to Endpoints’ Labeled A on the drawing
Now click on
to enter Draw line Between 2 Points.
Select the top point of the two long lines indicated by B and C. Please notice that the cursor
changes when it snaps to the endpoint of the lines. After the line is drawn the drawing should
look like the one below.
111
A
B
C
Draw horizontal line defined by length and using snap
Click on
values:
in the toolbar and enter the following
Line Length = -20
With the end point snap enabled. Select the end of
the short vertical line furthest to the right. This is
indicated on the picture below.
112
Draw Polar line defined by angle, length and using snap
Click on
values:
in the toolbar and enter the following
Line Angle = 180+45
Line Length = 5
With the end point snap enabled. Select the end of the
short horizontal line. This is indicated on the picture
below.
113
Chamfer the foremost corner
Enter the following values in the dialog that is already
open:
First Length = 2
Chamfer Angle = 30
Since the chamfer angle is different from 45 degrees
it is important to select the lines in the right order. The
angle will always be measured from the first element
selected.
So first select the vertical line marked A and then the
horizontal line marked B on the drawing below.
B
A
114
Draw a line defined by its endpoints
Click on
values:
in the toolbar and enter the following
First Point On Line Z = -20
First Point On Line X = 20
Second Point On Line Z = -40
Second Point On Line X = 20
Click on
to approve the command.
Now the drawing should look like the picture below.
115
Trim Between Points of intersection
•
•
•
Click on
to select Trim To Intersection.
Now Trim the long horizontal line. To do this select it as indicated with A on the picture below.
Now Trim the large circle. To do this select it as indicated with B on the drawing below.
B
A
116
Fillet intersections with radius 2.0
Click on
values:
in the toolbar and enter the following
Fillet Radius = 2
Select the elements on which the fillet operation
should be performed. This is done be left-clicking on
the part of the elements that you want to keep.
Select the elements as indicated on the picture below
by A and B.
Now you must select and left-click precisely on the
arc element you want to keep. This is the yellow arc
on the picture below.
A
B
117
Now repeat the process to fillet the additional radius 2 corners
Select the other two corners as A+B and A+C as shown at the picture below. Then select the
correct arcs to keep. At the end of the operation the drawing should look something like the
drawing below.
C
B
A
Now repeat the process for the fillet operations with radius 1 corners
First change the Fillet Radius in the dialog from 2 to 1.
Then you might want to zoom in on the area we will be working on as on the following
picture.
Then select the 3 corners as A+B, B+C and C+D as shown on the picture below. Then select
the correct arcs to keep. At the end of the operation the drawing should look something like
the drawing below.
118
A
B
C
D
Now the drawing is finished and it should look like the one below
Name the file and save it
Click on Files and then select Save as from the dropdown menu. Give the file a new name
and save it (the file extension is added automatically).
119
21. T
utorial 10
Machining the part
CNC-toolpaths
With CNC-Calc v2 it is possible to create toolpaths directly from the program’s geometrical
drawings. Thereby calculations become more secure and programming becomes much
faster compared to doing it manually. At the same time you get a big advantage since it is
possible to move, copy, rotate, scale and mirror elements with the result of instant NC-code
generation.
In the following we assume that the stock used are Ø60, and that it projects sufficiently from
the Chuck Jaws.
In order to produce the final part we will used the following operations:
•
•
•
•
•
•
Facing the front of the stock.
Roughing the part.
Grooving the areas that couldn’t be handled by the roughing tool.
Finishing the part.
Threading the front of the part.
Drilling the center hole in the part.
120
This tutorial demonstrates how the shown 2-dimensional part can form the basis of NC-codes
for various types of machining.
Note: This tutorial builds upon the result from the previous tutorial (Tutorial 9).
21.1.Before you start
The first thing to do before drawing a new part is to set the menu parameters. Start CIMCO
Edit v 5 and select Setup → Show Toolbars. Make sure all toolbars are displayed as shown
in the image below. Toolbars can also be displayed or hidden by right-clicking on the toolbar
area.
121
To make a new drawing you must click on
CNC-Calc and then select New Drawing.
Alternatively the same can be achieved by
clicking on the folder icon
in the toolbar.
Select the file from CNC-Calc Tutorial 9 and
click open.
You should now see the part from CNC-Calc v2 Tutorial 9 displayed in front of you.
Note: If you hold the cursor over an icon, for a moment, a short description of its functionality will appear.
122
21.2.Facing the front of the stock
To activate face turning click on the
icon. This will open the facing dialog to the left of
the drawing area. Insert the values shown below into the dialog.
Comment:
This comment will be shown in the final NCProgram. It is always good to include a comment, in
order to distinguish the various operations in the final
program.
Start Point Z: This is where the facing operation will
start along the Z-axis.
Start Point X: This is the start diameter of the facing
operation.
End Point Z: This is where the facing operation will
end along the Z-Axis.
End Point X: This is the end diameter of the facing
operation.
Now we have defined where the facing operation will work on the stock. This will be shown
on the drawing as a rectangle with arrows that indicate the direction of the operation.
Click the parameters button in the dialog to define how the operation will be performed.
Enter the following values shown below into the parameter dialogs.
123
Tool Orientation: The 9 icons represents the
possible 9 orientations of the tool.
Tool Radius: The is the nose radius of the tool.
Overcut Amount: This is the distance the tool
will cut longer than the Endpoint X value.
Roughing: Here the check-box can be used to
enable or disable the use of roughing passes. If
roughing is used each cut will be the size of the
Roughing Stepover.
Finish: The check-box can be used to enable or
disable the use of finish passes. If finish passes
are used Finish Cuts passes will be made with a
depth of the Finish Stepover.
Stock To Leave: The stock to leave is the amount
of material that will be left after the whole
operation is performed.
Compensation Type: This is the compensation
type that are used for the operation. The two most
commonly used are Controller or Computer.
124
Entry Amount: This is the length that the cut will
start each cut above Start Point X.
Retract Amount: This is the length that the tool
will pull free along the Z-Axis before it makes
moves for the next cut.
Use Entry Vector: Enable/Disable the use of
entry vector.
Entry Angle: The angle of the entry vector.
Entry Length: The length of the entry vector.
Use Exit Vector: Enable/Disable the use of exit
vector.
Exit Angle: The angle of the exit vector.
Exit Length: The length of the exit vector.
Click on OK to use the values.
Click on Show Toolpath, and the toolpath will be
shown on the drawing.
Try to experiment with the various parameters, in
order to see how they will change the generated
toolpath.
125
Click on Export to Editor in order to generate the actual program. Now a window like the
one shown below will appear. Notice that the comment from the dialog is inserted at the top
of the program as a comment.
In order to see how the program will run you can simulate this with the Backplot
functionality.
Click on
icon in the toolbar or select Backplot → Backplot Window from the menu.
Now a window like the one below will appears.
126
The Backplot animation is controlled using the slider and command buttons bottom right.
127
21.3.Roughing the part
To activate Roughing click on the
icon. This will open the Roughing dialog to the left of
the drawing area. Insert the values shown below into the dialog.
Comment:
This comment will be shown in the final NCProgram. It is always good to include a comment, in
order to distinguish the various operations in the final
program.
Retract Point Z: This is the Z value where the
operation will retract the tool to after completion.
Retract Point X: This is the Z value where the
operation will retract the tool to after completion.
The roughing operation work on a contour, and in order to generate a toolpath we must select
that contour. This is done by selecting the contour as indicated by A on the picture below.
A
128
When the selection is made the contour is selected until the end. This is OK for this operation
but we really don’t want any work done on the leftmost face so in order to exclude this press
the Back button once. This will deselect the leftmost face.
Now your drawing should look something like the one above.
Click on the Parameters button to open the parameters dialog. Enter the following values
shown below into the parameter dialogs.
Tool Orientation: The 9 icons represents the
possible 9 orientations of the tool.
Tool Radius: The is the nose radius of the tool.
Work Orientation: The four icons control the
way we machine the part. In the following we are
machining outside from right to left.
Horizontal Plunge: If the tool permit it we could
allow horizontal plunge.
Plunge Angle: Is the maximum angle we will
allow the tool plunge.
Compensation Type: This is the compensation
type that are used for the operation. The two most
commonly used are Controller or Computer.
129
Overlap: The distance that a cut will overlap the
previous cut.
Depth of Cut: The amount of material that is
taken in each cut.
Use Even Steps: Indicate what should happen if
the total depth is not dividable by the cut depth.
Should even steps be used or should the entered
amount be used.
Retract Distance: The distance that the tool
retracts from the stock before return move is
made.
Use Finish Passes: Should any finish passes be
taken.
Passes: The number of passes to take in the
operation.
Spacing: The depth of each of the finish passes.
Stock to Leave X: Is the amount of material that
will be left in the X-direction after the whole
operation is performed.
Stock to Leave Z: Is the amount of material
that will be left in the Z-direction after the whole
operation is performed.
130
Entry Amount: Is used to extend the toolpath
before it starts the actual cut.
Extension: Is used to extend the toolpath at the
end of the cut.
Use Entry Vector: Enable/Disable the use of
entry vector.
Entry Angle: The angle of the entry vector.
Entry Length: The length of the entry vector.
Use Exit Vector: Enable/Disable the use of exit
vector.
Exit Angle: The angle of the exit vector.
Exit Length: The length of the exit vector.
Click on OK to use the values.
Click on Show Toolpath, and the toolpath will be shown on the drawing.
Try to experiment with the various parameters, in order to see how they will change the
generated toolpath.
Click on Export to Clipboard in order to generate the actual program.
The program is now in the computers clipboard and is ready to be inserted into the CNC
program.
Change the window to the NC program, and move to the very end, by pressing Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit → Paste from
the drop down menu.
131
Now the NC program should look like the following screen.
In order to see how the program will run you can simulate this with the Backplot
functionality. Click on
icon in the toolbar or select Backplot → Backplot Window from
the menu. Now a window like the one below will appears.
132
21.4.Grooving the part
To activate Grooving click on the
icon. This will open the Grooving dialog to the left of
the drawing area. Insert the values shown below into the dialog.
Comment:
This comment will be shown in the final NCProgram. It is always good to include a comment,
in order to distinguish the various operations in
the final program.
Retract Point Z: This is the Z value where the
operation will retract the tool to after completion.
Retract Point X: This is the Z value where the
operation will retract the tool to after completion.
The Grooving operation work on a contour, and
in order to generate a toolpath we must select that
contour. To select the contour for the operation
perform the following steps:
•
•
Ensure that single step is checked in the Grooving dialog
Select the contour shown on the picture below. To do this start at the far right by selecting the R2 rounded corner with the indication arrow pointing to the left. Now select the next 2 element, so the selection looks like the one on the picture below
133
Now your drawing should look something like the one below.
Click on the Parameters button to open the parameters dialog. Enter the following values
shown below into the parameter dialogs.
Tool Width: This is the width of the tool.
Tool Radius: This is the nose radius of the tool.
Tool Orientation: The two icons indicates how
the tool is zeroed.
Stock Clearance: Indicates how far of the part
that the tool should move before making sideways
moves.
Stock Amount: How much stock is above the
actual groove.
Wall Backoff: If possible the tool will moe this
far away from the wall before it retracts.
134
Angle: This is the angle of the groves center line.
An angle of 90 degrees is a vertical angle on the
outside, while an angle of 0 is a horizontal groove
from the right..
Direction: This is direction in which the groove
is machined. It can be Positive, Negative or BiDirectional.
Stepover: This is the amount of material removed
in each cut.
Use Pecking: Indicates weather pecking is used
or not.
Pecking Depth: How deep should each peck be.
Pecking Retract: How far should the tool retract
between pecks.
Stock to Leave: indicates how much stock should
be left after the whole operation is performed.
Use Finish: Indicates weather or not finish cuts
should be performed.
Number of Finish Cuts: Describes how many
finish cuts that should be taken.
Cut Depth: This is the amount of material that
will be removed with each cutt.
First Cut Direction: The finish cut is made from
both sides. First Cut direction is the direction of
the first of the finish cuts.
First Distance: This is how far the first cut will
be taken along the contour.
135
Overlap: The second finish cut will overlap the
first finish cut by this distance.
Compensation Type: This is the compensation
type that are used for the operation. The two most
commonly used are Controller or Computer.
Click on OK to use the values.
Click on Show Toolpath, and the toolpath will be shown on the drawing.
Try to experiment with the various parameters, in order to see how they will change the
generated toolpath.
Click on Export to Clipboard in order to generate the actual program.
The program is now in the computers clipboard and is ready to be inserted into the CNC
program. Change the window to the NC program, and move to the very end, by pressing
Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit→ Paste from
the drop down menu.
Now the NC program should look like the following screen.
136
In order to see how the program will run you can simulate this with the Backplot
functionality.
Click on
icon in the toolbar or select Backplot → Backplot Window from the menu.
Now a window like the one below will appears.
137
21.5.Finishing the part
To activate Finish click on the
icon. This will open the Finish dialog to the left of the
drawing area. Insert the values shown below into the dialog.
Comment:
This comment will be shown in the final NCProgram. It is always good to include a comment,
in order to distinguish the various operations in
the final program.
The Finish operation work on a contour, and in
order to generate a toolpath we must select that
contour. To select the contour for the operation
perform the following steps:
•
•
Ensure that single step is unchecked in the Finish dialog
Select the contour shown on the picture below. To do this start at the far right by selecting the vertical line with the indication arrow pointing up. Now the whole contour is selected so unselct the last vertical line by pressing the Back button.
Now your drawing should look something like the one below.
138
Click on the Parameters button to open the parameters dialog.
Enter the following values shown below into the parameter dialogs.
Tool Orientation: The 9 icons represents the
possible 9 orientations of the tool.
Tool Radius: The is the nose radius of the tool.
Entry Angle: The angle at which the tool will
approach the part.
Entry Length: The length of the approach.
Exit Angle: The angle at which the tool will
retract from the part.
Exit Length: The length of the retract.
Compensation Type: This is the compensation
type that are used for the operation. The two most
commonly used are Controller or Computer.
Compensation Side: The side of the contour that
the tool will move on. This determines if it is an
inside or outside toolpath since the tool always
will move in the direction of the selection.
139
Click on OK to use the values,
Click on Show Toolpath, and the toolpath will be shown on the drawing.
Try to experiment with the various parameters, in order to see how they will change the
generated toolpath.
Click on Export to Clipboard in order to generate the actual program.
The program is now in the computers clipboard and is ready to be inserted into the CNC
program.
Change the window to the NC program, and move to the very end, by pressing Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit → Paste from
the drop down menu.
Now the NC program should look like the following screen.
140
In order to see how the program will run you can simulate this with the Backplot
functionality.
Click on
icon in the toolbar or select Backplot → Backplot Window from the menu.
Now a window like the one below will appears.
141
21.6.Threading the part
To activate Roughing click on the
icon. This will open the Threading dialog to the left of
the drawing area. Insert the values shown below into the dialog.
Comment:
This comment will be shown in the final NCProgram. It is always good to include a comment,
in order to distinguish the various operations in
the final program.
Start Z: This is the Z value where the operation
start.
End X: This is the Z value where the operation
end.
After the values have been entered in the dialog the screen will look something like the
picture below. Notice that the area of operation is shown with the blue rectangle.
142
Click on the Parameters button to open the parameters dialog.
Enter the following values shown below into the parameter dialogs.
Threading Type: The 4 icons represent thread
outside / inside made from laft to right or right to
left.
Thread Lead: Defines the starting position of the
thread.
Number of Starts: This defines how many starts
the thread will have, the normal is one.
Select From Table: Instead of typing all the
various values for the thread, these can inserted
from at table. These tables contains all of the most
common threads for both Imperial and Metric.
Please see below, for the use of thread form table.
Included angle: Is the total angle of the thread
profile.
Thread Angle: Is the forward angle of the thread
profile measured from vertical.
Major Diameter: Is the largest measure of the
thread.
Minor Diameter: Is the smallest measure of the
thread diameter.
143
Constant Area: With constant area the tool will
remove equal amounts of the area per cut.
Constant Depth: Using the constant depth
option each cut will have the same depth. Since
the removed area is triangular this will give an
increasing amount remover the deeper the tool
cuts.
First Cut Depth: The first cut defines how the
following cuts will be made based on what
method (Constant Area/Depth) is used.
Number of Cuts: If this option is used the
opeartion will be performed with this number of
cuts (+ the selected number of spring cuts).
Number of Spring Cuts: If spring cuts is used
the number of cuts will be made at the final depth.
Stock Clearance: Defines how far away from
the stock the tool should remove before it moves
back to the start.
Stock to Leave: How much stock should be left
at the end of the operation.
Pulloff Distance: Infeed Angle: Is the angle that
the tool will move down at. The reason for this is
to minimize the chip pressure at the front of the
tool and thereby obtain a more even thread.
144
Taper Type: If the taper angle isn’t zero a conical
thread will be produced. The two icons represent
the two ways the cone can go
Taper Angle: Is the angle of the conical thread.
Absolute Overcut: With this option the tool will
continue the defined distance at the end of the
thread.
Revelutions Overcut: With this option the
thread will be extended the number of revolution
entered.
Acceleration Distance is a distance that the
tool will start in front of the thread in so it can
accelerate in order to achieve a more uniform
thread.
Calculation Acceleration Distance: With this
option the acceleration distance will be calculated
by the operation.
Absolute Acceleration Distance: Here the
operator can enter the distance that the tool should
start in front of the thread.
Revolutions Acceleration Distance: With this
option the tool will use the given number of
revolutions to accelerate. It will therefore start
revolutions multiplied by the thread pitch in front
of the thread.
145
Click on OK to use the values,
Click on Show Toolpath, and the toolpath will be shown on the drawing.
21.7.Use of thread form table
In order to enter the form parameters for the thread it is possible to use Select From Table on
the Thread Form tab.
When this button is pushed the dialog below is shown.
The selection is the performed in the following way:
•
•
•
First select if the thread is a metric or imperial thread.
Based on the above selection the different types of threads can be selected in the drop down box.
It is now possible to select the specific thread in the list box, and when OK is pressed the form data will be filled out.
146
Try to experiment with the various parameters, in order to see how they will change the
generated toolpath.
Click on Export to Clipboard in order to generate the actual program.
The program is now in the computers clipboard and is ready to be inserted into the CNC
program.
Change the window to the NC program, and move to the very end, by pressing Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit → Paste from
the drop down menu.
Now the NC program should look like the following screen.
147
In order to see how the program will run you can simulate this with the Backplot
functionality.
Click on
icon in the toolbar or select Backplot → Backplot Window from the menu.
Now a window like the one below will appears.
148
21.8.Drilling the part
To activate Drilling click on the
icon. This will open the Drilling dialog to the left of the
drawing area. Insert the values shown below into the dialog.
Comment:
This comment will be shown in the final NCProgram. It is always good to include a comment,
in order to distinguish the various operations in
the final program.
Clearance Height: Is the position where the tool
is moved to before the actual operation and where
it will end after the drilling finished.
Retract Height: Is the distance from the start of
the operation where the feedrate will switch from
rapid to feed.
Start Depth: Is the depth at which the actual
operation is started.
End Depth: Is the final depth of the operation.
149
The Drilling operation is defined by the above parameters and after the parameters above is
entered the screen will look something like the one shown below.
The four entered distances are shown as the crosses on the drawing.
Click on the Parameters button to open the parameter dialog.
Enter the following values shown below into the parameter dialog.
Operation Type: The operation type can be
drilling or threading that is either Clock or
Counter Clock Wise.
Feedrate: Is the feedrate used for all feed moves.
Dwell: Is the time that the drill will dwell at the
bottom of each cut in order to break the chip.
Use Pecking: By selecting this option the
operation will be performed with pecking
movements.
Peck Clearance: Is the distance above the
150
previous cut to which the drill will move to in
rapid after the retract is performed.
Peck Retract: Is the distance the drill will retract
at each peck.
First Peck: Is the depth of the first peck.
Subsequent Pecks: After the first peck is
performed the entered distance will be used for
the remaining pecks.
Use Tip Compensation: Toggle the use of tip
compensation. This option is used for drilling
through a part. It will extend the hole based on the
geometry of the drill.
Tip Angle: Is the angle of the drill.
Drill Diameter: Is the diameter of the drill.
Tip Compensation: Is the calculated amount by
which the hole will be extended.
Click on OK to use the values,
151
Try to experiment with the various parameters, in order to see how they will change the
generated toolpath.
Click on Export to Clipboard in order to generate the actual program.
The program is now in the computers clipboard and is ready to be inserted into the CNC
program.
Change the window to the NC program, and move to the very end, by pressing Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit → Paste from
the drop down menu.
Now the NC program should look like the following screen.
152
In order to see how the program will run you can simulate this with the Backplot
functionality.
Click on
icon in the toolbar or select Backplot → Backplot Window from the menu.
Now a window like the one below will appears.
153
21.9.Tapping the part
To activate Tapping click on the
icon. This will open the Drilling dialog to the left of
the drawing area. It is the same operation that is used for both drilling and tapping. The
difference between the two is the parameters is the parameter dialog. Insert the values shown
below into the dialog.
Comment:
This comment will be shown in the final NCProgram. It is always good to include a comment,
in order to distinguish the various operations in
the final program.
Clearance Height: Is the position where the tool
is moved to before the actual operation and where
it will end after the drilling finished.
Retract Height: Is the distance from the start of
the operation where the feedrate will switch from
rapid to feed.
Start Depth: Is the depth at which the actual
operation is started.
End Depth: Is the final depth of the operation.
154
The Tapping operation is defined by the above parameters and after the parameters above is
entered the screen will look something like the one shown below. The four entered distances
are shown as the crosses on the drawing.
Click on the Parameters button to open the parameter dialog.
Enter the following values shown below into the parameter dialog. Notice that the dialog
is different from the one in the previous drilling operation. It is no longer possible to use
pecking because the Operation Type is selected as CW Tapping.
155
Operation Type: The operation type can be
drilling or threading that is either Clock or
Counter Clock Wise.
Feedrate: Is the feedrate used for all feed moves.
Depending on the machine this may be in a
different format. For this machines G32 code a
feedrate of 125 will actually result in a pitch of
1.25.
Dwell: Is the time that the drill will dwell at the
bottom of each cut in order to break the chip.
Use Tip Compensation: Toggle the use of tip
compensation. This option is used for drilling
through a part. It will extend the hole based on the
geometry of the drill.
Tip Angle: Is the angle of the drill.
Drill Diameter: Is the diameter of the drill.
Tip Compensation: Is the calculated amount by
which the hole will be extended.
Click on OK to use the values,
Try to experiment with the various parameters, in order to see how they will change the
generated toolpath.
Click on Export to Clipboard in order to generate the actual program.
The program is now in the computers clipboard and is ready to be inserted into the CNC
program.
Change the window to the NC program, and move to the very end, by pressing Ctrl-End.
Insert the text from the clipboard, either by pressing Ctrl-v, or selecting Edit → Paste from
the drop down menu.
156
Now the NC program should look like the following screen.
In order to see how the program will run you can simulate this with the Backplot
functionality.
Click on
icon in the toolbar or select Backplot → Backplot Window from the menu.
Now a window like the one below will appears.